True Position Calculator

What Is True Position in GD&T?

True position is a GD&T (Geometric Dimensioning and Tolerancing) control that defines the exact location of a feature (typically a hole) relative to datums. Unlike traditional ±X, ±Y coordinate tolerancing that creates a square tolerance zone, true position uses a circular (diametral) tolerance zone, providing 57% more usable tolerance area.

The true position value is calculated as twice the radial deviation from the nominal location: TP = 2 × √(Δx² + Δy²). This diametral value is compared against the tolerance specified in the feature control frame. A TP value less than or equal to the tolerance means the feature is within specification.

MMC (Maximum Material Condition) bonus tolerance is a powerful concept: when a hole is larger than its MMC size, the extra material provides additional positional tolerance. The bonus equals the difference between the actual feature size and the MMC size. This reflects the functional reality that larger holes are easier to assemble even with more positional error.

Formula: True Position = 2 × √(Δx² + Δy²) Δx = Actual X − Nominal X Δy = Actual Y − Nominal Y MMC Bonus = Actual Size − MMC Size Effective Tolerance = Stated Tolerance + MMC Bonus

Example Calculation

A hole nominally at (50.000, 30.000) measured at (50.12, 29.85) with tolerance Ø0.50 at MMC. Δx = 0.12, Δy = −0.15. TP = 2 × √(0.12² + 0.15²) = 2 × 0.192 = 0.384 mm. Hole is Ø10.15 (MMC = Ø10.00): Bonus = 0.15. Effective tolerance = 0.50 + 0.15 = 0.65. TP (0.384) < Effective (0.65) → PASS.

When to Use This Calculator

• An inspector is evaluating a CMM report and needs to calculate true position from measured X/Y coordinates to determine part acceptance
• A design engineer is determining whether to apply MMC or RFS modifier based on the functional requirements of a hole pattern
• Reviewing first-article inspection results for a new production part where bolt hole locations are critical for assembly
• Troubleshooting assembly fit issues by analyzing whether hole positional errors are within the allowed tolerance zone

Common Mistakes to Avoid

• Forgetting that true position is a diametral value (2× the radial deviation) — reporting radial deviation as TP understates the positional error by half
• Not applying MMC bonus when it is specified on the drawing — this causes good parts to be rejected; the bonus can add significant additional tolerance for oversized holes
• Using wrong datum reference frame — true position is always relative to the specified datums; using machine coordinates instead of datum-aligned coordinates gives incorrect results
• Comparing true position against bilateral tolerance — TP is a cylindrical (diametral) zone, not ±X/±Y; the two systems are geometrically different and not directly interchangeable

How to Interpret Results

• PASS with TP < 50% of tolerance: Excellent — the process is well-centered and capable
• PASS with TP between 50-80% of tolerance: Acceptable — monitor the process for drift
• PASS with TP between 80-100% of tolerance: Marginal — the process needs improvement to maintain consistent conformance
• FAIL: Part does not meet positional requirements — check datum alignment, machine calibration, and fixturing before rework or scrap decisions

Related Standards & References

• ASME Y14.5-2018 — Dimensioning and tolerancing (the primary GD&T standard)
• ISO 1101 — Geometrical product specifications — Geometrical tolerancing
• ASME Y14.5.1 — Mathematical definition of dimensioning and tolerancing principles
• ISO 5459 — Geometrical product specifications — Datums and datum systems

Frequently Asked Questions

Why use true position instead of ±X/±Y tolerances?

True position with a diametral tolerance zone gives 57% more usable area than the equivalent ±X/±Y square zone, reducing reject rates without loosening functional requirements. It also allows MMC/LMC bonus tolerance, which coordinate tolerancing cannot. Per ASME Y14.5, true position is the preferred method for locating features and is mandatory in most aerospace and automotive specifications.

What is the difference between MMC and RFS modifiers?

MMC (Maximum Material Condition) allows bonus tolerance as the feature departs from MMC — larger holes get more positional freedom. RFS (Regardless of Feature Size) means the tolerance is fixed regardless of the feature's actual size — no bonus is available. MMC is appropriate when the feature's function is assembly (clearance bolt holes). RFS is used when precise location is required regardless of size (press-fit holes, alignment pins).